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Plastic Part Design in SolidWorks

By Matt Lombard

Writing a set of rules that applies perfectly in all situations for design with plastic parts in SolidWorks is impossible. Below is a set of guidelines that I try to use when I'm working on plastic parts. Sometimes you have to bend the rules, and sometimes you have to throw them away altogether, but for most situations, these rules of thumb for plastic part design should serve you well.

Fillets cause many of the conflicts with other types of plastics features.

Fillet order, with respect to the other features, is critical.

Small convex fillets cause problems with shells, and any fillets between faces prevent multi-thickness shells.

Fillets running perpendicular to the direction of pull cause problems with draft.

Large fillets should be applied first.

Vertical fillets that can be tapered can go before the draft.

Fillets to be applied between the draft and shell:

Large, non-tapered fillets between faces of equal shell thickness.

Fillets to go after the shell:

Fillets with a radius smaller than the shell thickness.

Fillets between faces with different shell thicknesses.

Fillets that should not be transferred to the inside of the shell.

The most common cause for the shell command to fail is that there are fillets on the model that have a smaller radius than the thickness of the shell.

Use Tools, Check to find minimum face curvature, geometry errors or short edges.

Severely sharp, pointy geometry may also frustrate the shell.

Cut away sections of the model that look suspicious and retry the shell, then narrow in on the problem area.

Existing bad geometry may cause a shell to fail for no apparent reason. Use Tools, Check to find bad faces or edges.

It is recommended to add small fillets after the shell.

Draft can come before or after shell. Remember that if it comes after, you will also have to draft all the interior faces.

Drafting a face that is adjacent to a fillet that runs perpendicular to the direction of pull will not usually give acceptable results, even if the feature does not fail.

All tangent faces should be drafted the same amount.

Be aware of how draft changes the wall thickness of parts.

Draft is sometimes not required on faces that will pull away from the mold due to shrink. It is always best to consult the tooling engineer before doing this.

Drafting a fillet running parallel to direction of pull results in a tapered or variable radius fillet. The alternative is to apply the draft before the fillet.

Draft features can be applied to faces which already have draft on them (draft is not “cumulative”).

Draft can even be applied to straighten out curved faces when axis of curvature is perpendicular to direction of pull.

Scale should be added to the engineered part as a separate configuration.

Scale does not change the size or position of sketches or planes.

In assemblies, avoid making in-context references or mates to unfinished plastic parts, unless you are sure that the face or edge being referenced is not going to be consumed later by a draft, fillet or split line feature.

Mates to drafted plastic parts may be best handled with planes.

About the Author

Matt Lombard received a bachelor of science degree in mechanical engineering from Rochester Institute of Technology. He has written and presented numerous SolidWorks classes, and served as a consultant and trainer in plastics design for such companies as Fisher-Price, Rubbermaid and Hamilton Beach/Proctor Silex. He is also the founder of the Rochester User Group for SolidWorks. For more SolidWorks tips from Matt, visit his website at: http://www.frontiernet.net/~mlombard/.

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